Getting Started with Inventor Model States

Share this Article

Model states were introduced in Inventor 2022 and enable you to save configured states of components (parts and assemblies). They can be incorporated into your designs for many uses, including helping to optimize assembly performance, reducing the clutter of large numbers of components, or in the case of part design, creating a model state for manufacturing or FEA analysis.

Model states have multiple uses within part and assembly files. Uses can include creating manufacturing stages, simplifying the display of an assembly for design work, or creating configurations of components in a design to represent various products. Model states can also be valuable when working with a large assembly to improve retrieval times and performance, or they can be used as a starting reference for model simplification. The model states shown in Figure 1 are examples of model states for part (top) and assembly (bottom) files.

Figure 1
Figure 1. Examples of model states for part (top) and assembly (bottom) files.

Creating Model States

The process to create model states in parts and assemblies is similar. The following steps describe the process:

How to Create a Model State

1. In the Model browser, right-click on the Model States node and select New. Alternatively, you can right-click on the model state you want to copy and select Copy. The model states, as shown in Figure 2 for a part and assembly, were created as a copy of the active Master model state and and are immediately activated once created.

Figure 2
Figure 2. Model states for a part and assembly.

2. Verify the edit scope setting is appropriate for the model state customization that you will be doing. This setting determines if the change will affect only the active model state or all model states. By default, the edit scope is set for the current model state only and the blue pencil icon appears adjacent to its name.

  • By enabling the scope to affect all model states (as shown for an assembly in Figure 3), you can ensure the change is made to all model states. When enabled, the blue pencil icon appears adjacent to all model state names, indicating they will all be edited.

  • Scope editing functions the same in both parts and assemblies.

Figure 3
Figure 3. Enable the scope to affect all model states.

The Delete operation is global and affects all model states regardless of the edit scope setting. To delete a feature or component from a model state, you must activate it and set it as suppressed.

3. With the new model state active, modify the configurable attributes for the part and assembly as follows to customize the model state. Once modified, each configurable attribute is assigned a column in the file’s internal model state spreadsheet.

  • Suppress/unsuppress part or assembly features in the model state.
  • Suppress/unsuppress components in the model state. Note: The bill of materials will list suppressed assembly components as a QTY 0.
  • Modify the iProperties, as required, for the active model state. In the Model browser, right-click the model state name or the model name and select iProperties.
  • Materials can be assigned to model states at the part level. To incorporate a specific part in the top-level assembly model state, the required part-level model state can be enabled as required.
  • Modify parameters, as required, for the active model state. This can be done in the Parameters dialog box ( ) or by showing dimensions in the graphics window and modifying them.
  • In the Model browser, modify constraint offset values, as required, for the active model state.

4. Rename the model state using a descriptive name by clicking it twice (not double-clicking) in the Model browser and entering the new name.

5. (Optional) Once you have created one model state, you can use standard spreadsheet functionality to create additional model states or add customizable attributes. To open the spreadsheet, right-click on the Model States node in the Model browser and select Edit via Spreadsheet. Edit as required, save, and close. The model states update to reflect any new model states or edits to existing model states.

6. Save the file to save the new model state.

You can make changes to the model states once created. To do this, ensure the required model state is active, verify the edit scope setting is as required for the change, and manipulate them as needed. Once edits are done, ensure the file is saved.

Model States in Subassemblies

Subassembly model states can be enabled within model states in the top-level assembly. In these situations, the model state must already exist in the subassembly. You cannot create, edit, or delete subassembly model states within the context of a top-level assembly (in place edit). To do this, you must explicitly open the subassembly in its own window to create/edit. For example, the Screw_Sub subassembly shown in Figure 4 is active in the context of the assembly. The right-click model states menu does not allow you to create a new model state.

Figure 4
Figure 4. Screw_Sub subassembly.

Model States Versus iParts/iAssemblies

The model state functionality was introduced in Inventor 2022. It is a replacement for the pre-2022 level of detail assembly functionality, and additionally provides an alternative to the iPart and iAssembly functionality (still available in Inventor 2022). With the introduction of model states, the model state functionality and the iPart/iAssembly functionality become mutually exclusive. The model state functionality is enabled by default in all new parts and assemblies. If you are using previously created files, consider the following:

  • If the file does not contain pre-existing iParts or iAssemblies, the model state functionality is enabled. Any level of detail representations that existed (assemblies only) are converted to model states in Inventor 2022.

  • If the assembly contains pre-existing iParts or iAssemblies, the model state functionality is not enabled. Any level of detail representations that existed (assemblies only) are converted to design view representations in Inventor 2022.

The process of converting an iPart or iAssembly table that exists in a pre-2022 assembly to model states is manual. You can either delete the table and recreate the configurations using model states or you can use spreadsheets, as follows:

1. Open the file, right-click on the Table node in the Model browser, and select Edit via Spreadsheet.

2. With the spreadsheet open, copy the data or save the file to a temporary location.

3. Delete the iPart/iAssembly table. A Model States node appears in the Model browser, indicating that it is active.

4. Create a new model state in the file.

5. Right-click on the Model States node and select Edit via Spreadsheet.

6. Copy the data from the iPart/iAssembly table into the model states table to provide a starting point for your model states table.

Note that the syntax is not the same in the two tables. For example, model states tables use Compute and Suppress for feature/component inclusion and iAssembly tables use Include and Exclude. Edits will be required for the model states table to be recognized and generate the required configurations.

Consider the following:

  • Unlike iParts and iAssemblies, model states are all saved and managed in the one part or assembly file.

  • To return to iAssembly functionality, only a Master model state can exist in the file. To switch, on the Manage tab, click (Create iAssembly) and create an iAssembly member. Once complete, the Model States node is removed from the Model browser and is replaced with an iAssembly table.

Model States and Autodesk Vault

Model states offer capabilities similar to those found in iParts/iAssemblies; however, all configurations are stored in a single file instead of multiple files. Additional Vault integration functionality is available for model states if your Vault Professional implementation includes items. If your Vault implementation does not include items, any file that contains model states will display the master model’s properties (e.g., iProperties, parameters, etc.). If you require separate files that can be managed and released, consider using iParts and iAssemblies. For more information, see “Working with Model States and Vault Files” in the Vault Help documentation.

Substitute Model States

A substitute model state enables you to swap out a complex component for a simpler one that represents it. The substitute still contains all of the BOM information that is normally associated with the assembly, as well as the physical information (such as center of gravity and mass). Using substitute parts reduces the amount of components loaded into memory, as well as the number of constraints and adaptive relationships that must be recalculated when changes are made. By simplifying the model, the intention of a substitute model state is to reduce the computing resources and thereby increase performance without sacrificing access to BOM information.

The model on the left in Figure 5 shows the Master model state for an assembly. A substitute model state for the fan and its electronic components is shown on the right. In this example, the substitute part was simplified using a simple cylindrical-shaped part; however, substitutes can also generate a part file with surfaces or merged solid bodies to help make the substitute model state simpler to help improve performance.

Figure 5
Figure 5. The model on the left shows the Master model state for an assembly. A substitute model state for the fan and its electronic components is shown on the right.

Create a Substitute Model State

1. Open the subassembly that is to be simplified. This assembly is called the Owning Assembly.

2. (Optional) Create a reduced-part model state for the subassembly. In this model state, suppress any subassembly components that can be removed to help further simplify the assembly. This is not a requirement.

3. In the Model browser, right-click on a model state node and expand New Substitute. Select one of the options shown in Figure 6.

Figure 6
Figure 6. Option selection.

  • The Derive Assembly option simplifies the assembly using the Derived Component functionality. A new part file is created that is then substituted for the assembly in the model state. The derived part is created in the same way as one that uses the Derive tool. You define its name, template, and location, and then use the Derived Assembly dialog box to control which components are included in the new part file. The new substitute model state is created using the new derived part file.

  • The Simplify command creates a simplified substitute part that represents the active assembly and uses that part in a substitute model state. The simplified substitute part is created in the same way as one that uses the Simplify tool. The new simplified substitute part is automatically created, and a substitute model state is created that uses it.

  • The Select Part File option substitutes a single part file for the assembly. Selecting Select Part File substitutes a selected file for the assembly in the substitute model state. The part file can be a previously simplified assembly, simplified model, or another part file. After you select this option, you are prompted to select a component. The substitute model state is created using the selected part file.

4. In the main assembly, create a new model state and activate the substitute model state in any subassemblies, as required.

Tip #1: You can also create a simplified substitute model (with a substitute model state) by clicking Simplify in the Assemble tab> Simplification panel and setting the Substitute type in the Properties panel.

Tip #2: Individual parts cannot be simplified. To create a simplified part of a specific subassembly inside the top-level assembly, you must first open the subassembly explicitly (it cannot be edited and created in place) and create a substitute model state in that assembly. After saving and returning to the master subassembly, the lower-level model state is available for selection in the higher level’s Model States folder.

Using Model States in Drawings and Presentations

Drawing Views

Any model state can be selected for use while creating base drawing views. When modifying the parent view, you can also change the model state that is active by editing the view. When creating a base view, select the required model state name from the drop-down list, as shown in Figure 7. To change the model state that is used in a base view, right-click on the view, select Edit View, and select a new model state name. All views that reference it will also update. Hint: If you want an isometric drawing view to have a different model state than a 2D base view, create the isometric view as a new base view and orient it as needed.

Figure 7
Figure 7. Select the required model state name from the drop-down list.

Assembly Parts Lists

Drawing parts list tables must be associated with a view when created. If the view has been set to represent a model state, the parts list will reflect this. If components are suppressed in the model state, their QTY value will report appropriately. If a component does not exist in a model state, it will still show the component as an item and will have QTY 0.

Figure 8 shows a drawing sheet with two different model states documented. The 2D views show the parts list with one vise assembly. The isometric view’s parts list shows all four vise components included.

Figure 8
Figure 8. A drawing sheet with two different model states documented. The 2D views show the parts list with one vise assembly. The isometric view’s parts list shows all four vise components included.

General Tables

A general table can be used to show all of the model state details for a drawing model’s configurations. To create this table, complete the following steps:

1. Click (General Table) on the Annotate tab to open the Table dialog box.

2. Select the drawing view that will be the source for the table. The view can be the master or a model state configuration of the assembly.

3. In the Columns and Rows area, select (Column Chooser).

4. In the Table Column Chooser dialog box, select the columns that you would like to include in the table from the Available Columns list and move them to the Selected Columns list using the Add option. The list will include all of the configurable items that were modified in the model states (e.g., dimensions, parameters, components, etc.).

5. Click OK twice to create the table and add it to the drawing.

6. (Optional) To customize the column names, double-click on the table to edit it, right-click on the column name, and select Format Column. In the Format Column dialog box, you can disable the Name From Data Source option and enter a custom name for the column.

Figure 9 shows the columns that were added to the general table for a part and the resulting drawing table that was created. In the table, the column headers were customized to have descriptive names using the procedure described in Step 6 above.

Figure 9
Figure 9. Columns that were added to the general table for a part and the resulting drawing table that was created.

Consider the following when working in a drawing with model states:

  • If a design change is made to a model state that is used in a drawing view, it will update to reflect the change when next opened. Any associated parts lists or general tables will also update.

  • The model state assigned to a view can be switched by editing the view and selecting an alternate in the Model State drop-down list.

  • A view can be modified to replace its reference model (and its model state) using the (Replace Model Reference) option on the Manage tab. In the Replace Model Reference dialog box, select the file that is being replaced, select , select a new file, and click Options. In the File Open Options dialog box, select the required model state. Once the file is replaced, the view and associated parts lists will update.

  • If a substitute component is used in the model state to represent an assembly, it is still identified as a single item to provide an accurate BOM and parts list.

Want more? Download the full class handout. 

For the past 25 years, Jennifer has been teaching and developing CAD training material for both a synchronous and asynchronous learning environment. She is currently working with the Rand Worldwide company, ASCENT - Center for Technical Knowledge, where she develops and manages the training curriculum used by Autodesk Authorized Training Centers. She also has her Autodesk Certified Instructor (ACI) certification. Jennifer MacMillan holds a mechanical engineering degree from Dalhousie University, Nova Scotia, Canada.